View Full Version : plunge roughing techniques?

10-22-2006, 04:03 PM
Hey all,
I have used plunge roughing once just to see how it works. I had part recently that had a narrow deep (2.5") pocket with .1875 rads in the corners. I thought plunging would be better than a long skinny rougher. problem is the plunging starts in the middle of the part instead of the edge where I would like it. Does anyone here know if you can get surfcam to start plunging on the edge instead of the center of the material?


Tony the Ferret
12-06-2006, 10:04 AM
Think you should give your local Sescoi offices a ring, they have had plunge roughing for years, great way to remove material

12-06-2006, 09:43 PM
thanks for the really helpful reply, tony.

12-06-2006, 09:55 PM
Well what you can do is create four point at the corner you want the plunge and create toolpath for that(like drill cycle) before other toolpath you are talking about.

12-08-2006, 10:27 PM
hi, i like what the first 2 posters have to say, and maybe i dont understand what your doing, Im kinda with NewTexas, as i would drill out the corners and reduce endmill sizes. perhaps innefficient. so that said, since i dont really know what your doing, let me suggest this.

do you know about DR drills? fantastic insert life. coolant thru not required. its a centercutting drill. insert based. and wow we love them, we have 3/4 to 1.5" and they rule, ive been begging for a 2" and they wont give it. i think its a holder issue, but i dont understand cause we use the ungodly heavy 50 series holder.

12-10-2006, 01:25 AM
it is an "open" pocket with .1875 rads in the corners but it is 3 inches deep. the open side was on the right. With plunge roughing it's not exactly the same as drilling, because you are not plunging with the full diameter of the cutter, you are only plunging with the radius of the cutter or less and stepping over the same amount for the next plunge. If I could start the first row of plunges on the right edge of the material I would never be taking a full diameter cut. which is what I was trying to do. Surfcam was starting the plunges in the center of the material where it would take the first plunge as if it were drilling, and probably destroy the cutter right off the bat because there is nowhere for the chips to go.
Most of the toolpaths in surfcam let you pick a plunge point. I just couldn't find a way to control this plunge point with plunge roughing. I talked to the engineer and we change the design so I could wire it out on the edm. if I can remember I will try to post some screenshots to make it more clear what I was trying.


12-10-2006, 11:29 AM

How about drilling a plunge point? You could pretty much drill it where ever you like an go from there, couldn't you? I haven't used the technique yet, but I have a job coming up using a tough material that's a mixture of nickel, tungsten and some other stuff, and it's a bear to cut. The first part was made from brass while we were waiting on the denser material to come in, and I just used a Z-level roughing operation with a spiral engage, but I don't think I'll get away with that on the next part. I'll be watching to see what you think of plunging.

Tony the Ferret
12-10-2006, 05:26 PM
Sorry, i thought this was a serious request for "plunge roughing" not "chain drilling" this picture is what we call plunge roughingThis block is about 12" X 8" and the plunge depth was MAX 3", this was done AUTOMATICALY, we did not drill any start points, or tell it the start position, Although WorkNC would need to for a closed "cavity" situation. WorkNC can also do the "chain drilling type" for profiles & pockets to points or follow curves

12-10-2006, 08:52 PM
Tony, go back to the first post and you will see that the question was regarding a cavity plunge rough operation. That's why the pre-drill was mentioned. Also, this is the Surfcam forum, and yes Surfcam I'm sure would plunge rough the part in your picture quite well. I know WorkNC is a great program, but I doubt that the OP has it.

12-19-2006, 12:09 PM
create a point at one end of slot / pre-drill first!!
then go to your plunge mill, array tool path for
the no# of plunges you will need to complete your slot.
keep your plunge moves no greater then radius of tool
apart or less.

02-01-2007, 01:58 PM
I understand you want to plunge rough material that is a open ended slot, you will need to make a simple addition to the existing geometry but it is simple. To get plunge rough to start on the out side of the part create an offset material line that will replace the existing material line then link the new line to the existing slot element ends, use half the diameter of the cutter for the offset value. Go to the plungerough, pick the surfaces and then pick the boundary (including the new entry lines), a small window pops up set Boundary type, material height and then set “Tool Center” to “Before boundary” and the “Boundary is” to “Tool Containment”, these settings force the tool to be inside the boundary chosen – that is why the offset line was made outside of the actual stock, to allow for the tool to start in a open area. To get the tool to start on the open end of the slot choose two endpoints on that new line that you created, note that you may need to pick them in the opposite direction to get the cutter starting on the open end of the slot, I am not sure why, it just works that way. The settings I choose for the cut control page were “Grid type = Square”. Hope this helps

02-05-2007, 07:11 PM
Good answer camaru I will try that. The part in question was put on the back burner for a while so I will be machining it in the near future.